Bridges & Tabs - which one is the final say?

[knedert]

Been lurking about using the search function, but not finding the easy answer. So here it goes...

Have successfully created bridges on 2-D profile cuts.
Send file to SB, and wonder about the Yes or No for tabbing in the fill-in sheet.
Have always clicked the Yes, because my logic is "Yes I programmed them, Yes I want them."

Too chicken to click the No button.
I *think* that the SB program is adding tabs - but not sure...
We may have other bigger issues with our table not being perfectly flat.
Currently holding down the .5 inch material with brass screws strategically placed *out of the way*.

So to sum my question up: Can I program the bridges in, and click NO on the tab fill-in sheet before pressing the big START button?

Thanks in advance!
Rose

[3d_danny]

If you have created the bridges within your cut file, then using the SB tabbing feature will add more tabs. When you have the parameters sheet open, look towards the bottom on that page and you will see "VB-to set TaBbing Values". You can set the distance between tabs, length, height, etc.

If you keep the default Tabbing set to off, then you will only cut your file with your bridges.

Dan

[knedert]

Well... that does explain those mysterious lumps left over in the area clear tool path!
Next time I'll be brave and trust the bridges only.
Thanks!
Rose

[paco]

Previewing toolpath first (before launching the tool) might make you feel more secure...

[knedert]

Can I highjack my own Topic and ask something about 3-D? If not, where should this go?

Situation: Created relief from vector art, then using 3-D relief toolpath, hogged out the majority with a 1 inch ballnose bit. Followed with an 1/8th inch ball nose for the detail.
Ran the whole thing with the 'Bot on .5 inch MDF.
Was very pleased with the results of our first 3-D work.
HOWEVER.....
there were a couple sections of the piece that the 1 inch bit nicked out of the finished piece.
At first we thought it was machining error.
But then I looked at the simulation again - running it backwards: detailed toolpath first - looked good then ran the 1 inch bit toolpath and Blammo! There was the nick - exactly where it was in real life!
Okay - so we learned that it was software induced - not hardware. That helps. The 'Bot did *exactly* what it was told to do.
Therein lies the problem.
When I created the 1 inch toolpath to hog out the majority of the work I used .03 inch in both the allowance and tolerance. What could I have done to prevent these nicks. There are only 2, but still there should not be Any.

I have tons of other questions, but have a hard time trying to describe them to myself - much less you all! Thanks for bearing with me.
Rose

[paco]

Rose,

if it's nicking sideway details, I say you need a smaller roughting tool bit than a 1"... a 1/2" CED would be still fast I believe for most project... unless it's VERY large.

Is it's nicking down and should'nt, it has to do with the toolpath to CAD design bounderie; the toolpath is machining a little outside the CAD goemetry, hence it try to machine the side(s) of the geometry.

If you got a pic, maybe we can clear this out right away...

What 3D CAM are you using? I had this "problem" sometime in MeshCAM; not really a problem but rather a added setting!

Hijacking thread at TSB is quite common...! Not a problem if you ask me.

[knedert]

Paco,
It's nicking sideways. So will try a smaller bit next time. The entire hog out area is less than a foot wide. Time is not so much a factor for us at this time, the devil is in the details!
Would love to send a picture - but for 2 things: 1) Am I really limited to 50 x 50 pixels?
2) My Photoshop CS has been hanging up on launch for the last couple of months and it's doing it again. I haven't figured out what it is that hangs it up. Grrrr.......
So, back to vector wrangling and welding for fun!
Rose

[billp]

Rose,
As Paco points out that's a pretty large bit for roughing out, AND in many cases using a ball nosed bit for the rough out does not work as well as a flat bottomed bit. In fact in some programs when you do a simulated toolpath the projected cutting time will be huge because it is reading only the tip of a ball nosed bit rather than the full diameter. You might try a .5 " flat bottmed bit for your rough out and see what the results are...

[paco]

Rose (and all who got problem with TSB pics and screen shots),

try this (it's free, already at the reach of your fingers and still quite fast); on your keyboard,

-push the 'Print screen' button (upper right most on most keyboard)

-start MS Paint

-paste the current content of the clipboard (Edit/paste or CTRL+V)(when one push 'Print screen', this copy the entire screen of your PC), this will create a new image based on the screen shots you've just picked...

-with the select tool, select what you want to keep (don't select too much; you're limited to 400 X 400) and copy (or cut) it to the clipboard (Edit/copy (or cut) or CTRL+C (or +X))

-then clear the current image to a max of 400 X 400 (Image/Clear Image) and resize the canvas (I like to use the lower right control /black dot to do that fast, dragging it upper left for a really small canvas)

-Paste your copied selection the resized canvas and save it on your desktop (I suggest as JPG for size of file)...

You should have a ready to post pic! Normally this process get correct file images but if your file size is still to large (even if your image is'nt larger than 400 X 400), you'll need an image software to save it to a lesser resolution (or resize the image until it's small enought in term of file size). How about The GIMP! (http://www.gimp.org/)

[knedert]

Thanks Doc.
That should solve the problem of the leftover tooling outside of the final area that I used the smaller bit on.
Since it was the first (Yipee!) 3D we'd done, we were pretty darned pleased with getting anything!
Here's my first attempt at posting pictures:

5188

5189
Lots of Firsts going on here!

[knedert]

Hey Paco,
Thanks for the tip -
While you were posting it I somehow got Photoshop working again.

There are some of us old Mac users who have switched to PC - that keep a handy 10 foot pole between us and as many MS products as possible (think Word, Excel, Paint)
While this has been limiting at times, it sure does slow down on the non-documented operating features! tee-hee
Rose

[Brian Moran]

Rose,
You say ...
> I used .03 inch in both the allowance and tolerance
You didn't answer Paco's question about which software you were using, but for many packages these values will not make sense.

The allowance field is usually used to specify a 'skin' of material left on all over the model. The tolerance field says how far the toleranced toolpath can deviate from the original toolpath - both PLUS and MINUS.

So by entering the same value for tolerance and allowance, the toleranced toolpath can still deviate far enough to JUST come into contact with your original surface. This is not usually what is desired when leaving an allowance so the tolerance should be a fair bit smaller than the allowance.

This information may not be true of all machining packages, but is certainly how these fields are interpreted for instance by ArtCAM.